Page 1 of 2 12 LastLast
Results 1 to 12 of 20

Thread: CNC lathe tool and work offsets

  1. #1
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default CNC lathe tool and work offsets

    I could use some help setting up my cnc lathe. I've worked with Machining centers for a long time, but am new to lathes. What I am having trouble with is - how do you set x,z zero for the work offset (i.e. G54) ? I have heard some comments about using a reference tool, but do not understand it completely. Just about everytime I have programmed a mill, I set the x,y zero to the part zero then touch off all the tools in Z and ready to go. Lathes aren't the same, obviously. The machine we have is a Daewoo Puma 6-HS with the Fanuc 10T. Any help and insight will be appreciated.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Jun 2005
    Location
    USA
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default

    This is the method I use to touch off tools, hope it helps. At home or reference position origin all. Look at the incremenal position numbers, they should be zero. Move the tool to the part and position tool at z 0.0 on the part write down that number. take a cut on the diameter write down that number, measure the part and add to the x number. Use theses numbers in a g50 line at the beginning of your program. Your tool offsets will be zero to start and you can make small adjustments from there.



  3. #3
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default cont.....

    That is sort of the same way I go about starting out on mach. centers. First I home the machine and then set the absolute position for x,y to zero. I usually do this by setting the offset in G54 to zero and then MDI input the G54 X0 Y0. With no move commanded, this just changes the displays for x,y to zeros. Then I go find part zero (edge finder, indicator, etc) and whatever the display reads is what goes in the G54 offset. I would like to do the same thing with this lathe, but after homing I MDI input the G54 X0 Y0 with no G1 or G0 and the machine started moving - much to my surprise. After hitting feed hold and reset, I went and checked the G54 offset and X, Z were both set to zero. Can anyone explain, first off why the axis movement with no G0 or G1 commanded? Secondly, I understand the concept of touching off the tool in Z, but I need more clarification of the X after taking skim cut. The measurement of dia. after cut - does this number go in the G54? Also, I am assuming the tool to use is the first tool - which would then be sort of the reference tool ?? Are the rest of the tool offsets then set from this reference ?? I will be setting this lathe to run 4 different parts and would like to use the G54, 55, etc. for each part. Maybe I shouldn't be stuck in this mode of thinking but I like to keep things consistant.



  4. #4
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    The way I've got it figured, every machine establishes its home position after doing the reference point return, which is normally executed shortly after powering up the control. The home position is based in G53, which is called the "machine coordinate system".

    You can change coordinate systems by calling them by their name, G54, for instance. An X, Y or Z value with the G54 will do nothing, unless the machine is already in G01 or G00 mode from a previous command. True, it does "reset the displays to zero", as you said, but no motion occurs on your mill, because you have simultaneously called the G54 coordinate system, and then commanded a zero move within it.

    Certain lathe controls may invoke either G01 or G00 mode automatically, from a parameter setting which is read at startup.

    Now, on a mill, the Z axis G53 home position is typically "up" somewhere near the top of the stroke, and it will have an assigned value of Z0. On a lathe, the G53Z0 might logically be placed somewhere near the face of the chuck. G53X0 would logically be placed along the spindle centerline.

    So, when you command the lathe to G54 X0 Z0 (with only zeros in the G54 table), it sees that there is no difference between the G53 and G54 coordinate systems, that is, they coincide exactly. Because G00 or G01 mode is "on" by parameter perhaps, it begins a movement to that position. So, that explains why the lathe begins the movement. It would be interesting to know where G53 X0Z0 really is on your machine. You should be able to determine where this is, by what the displays readout, as soon as the machine is homed after power-up.

    On a lathe, the position that the tool turret takes when the machine homes is basically at a random location relative to what I would call a "logical" reference point on the machine. On a lathe, the spindle centerline is all important, so that is definitely logical to call the centerline X0 in the G53 coordinate system. The chuck face makes a logical Z0 in the G53 coordinate system, too, but there could be other positions that the machine maker set up to serve as G53Z0. Every machine might use different chucks, or whatever, so the factory may opt to use some other Z0 reference.

    When the tool turret is sent to "home" on a lathe, it does not return to G53 X0Z0, because, as you have discovered, the position may be inaccessible. But on a mill, all the axis do return to G53 X0Y0Z0 because the position is accessible.

    Instead, a lathe uses a predefined point called a G28 position, which is based off the G53 coordinate system. Parameter settings in the lathe setup, define what the G28 position is. It typically places the turret somewhere out in front of the chuck, back off of the X axis far enough so that turret rotation will not cause a tool to hit the workpiece. Typically, the X axis will retract far enough to stop just short of the X+ overtravel limit switch.

    G00 G28 alone will cause the turret to move to this stored position. If a value is commanded with the G28, then the turret will first move to that commanded value, and then to the home position, a dogleg sort of movement. Many guys forget that an XZ value with a G28 is an intermediate position. This is why it is common to see G91 G28 X0Z0 because then the intermediate point is incrementally "zero" away from the current position, so then the machine returns straight to the G28 stored position. On lathes, it is common for a U and W value to be interpreted as an incremental movement (no G91 required), so a lathe command might be G28 U0W0. The reason it is done this way is that you don't have to remember to set the mode back to G90, which could be a problem. But, I digress from the discussion

    Now, for your reference tool problem. You would need to know if the controller has automatic calculation of the offset, and how to make it store the values.

    When the G28 position was set up in parameters in your machine, it would make the most sense to have them correspond to the datum point of an external finishing tool, in pocket #1 of the turret. This is what I did when I set up my machine. I took trial cuts, using the display values of the G53 machine coordinate system. I determined by trial measurement, how to adjust the G28 X parameter so that it actually corresponds to the real position of T#1, relative to the part centerline. This may seem kind of a$$ backwards, but once its done, its done. Now I know that for this reference T1, the X tool offset will always be very near zero. Any other tools that I might use, if they cut the correct diameter, then their offsets are automatically "related" to T#1, because T#1 is correctly set in the machine coordinate system.

    The Z offset for T#1 is not as unambiguous. The operator needs to determine what he will always use for a Z reference. Since I use one chuck on my lathe, I use its face for a reference. Again, I touch off the chuck face with T#1, and note the display coordinates in the G53 machine coordinate system. This should read Z0. If it does not, then the G28 Z parameter needs to be adjusted until it does. The goal is to make the Zoffset of T#1 = 0, and to remain this way, perhaps with wear offset or tip radius offset being the only adjustments ever made for the Z offset of T#1.

    Now, I touch all other tools off the chuck face, and they are all related to T#1 automatically.

    With this system, you should be able to machine without using G50 fictitious work offsets. The G50 is akin to the old G92 used on the mill, which has a certain danger associated with it.

    And, when you wish to put a part of any length in your chuck, the G54 offset only needs a Z value, and this value equals the distance between the end face of the stock and the chuck face, if that is where your Z0 reference in G53 is located.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  5. #5
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3086
    Downloads
    0
    Uploads
    0

    Default

    Guys

    I, as well, am familiar with using a VMC (my way ;-)) and have just purchased my first simple CNC lathe (Fagor 8040T control).
    I am in the process of figuring things out and getting some training.
    Hu - fairly impressive and confusing post, the water started to clear about 3/4 of the way through. It sounds as though you do a lot of 1-offs (as I do) and set the machine to be versatile and easily set for the next part.
    Can fixture offset not be quickly set as well be touching or skim cutting the virgin stock and inputting an offset zero? (Such as you would do on DRO?) Similar to what DMayfield is saying only without all the calculations?

    www.integratedmechanical.ca


  6. #6
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Darebee,
    I don't claim that my way is the only way You feel free to explain alternative methods.

    I derived the logic for my method on my own. I got tired of working with coordinate system offsets that had no useful relationship to the machine. You think that was confusing, well, I couldn't ever explain the way I used to do it before that A person can always find some kind of a method that works, but whether it makes sense, is another matter.

    I changed methodology to get away from using the G50 (aka G92 on mill) method of creating a coordinate system.

    All the calculations I described are a "one time" deal. They have everything to do with initial setup of the machine and the reference tool. Once the reference tool position is accurately described by the displays when the tool is at home, the rest of the settings are child's play.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  7. #7
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default

    Hu -
    Thanks for the reply, a very good logical one I might add. I like the idea of setting up the machine from known logical coordinates and the reference tool - I am just not sure how to get there from where I am at with this machine. Did some checking of how the machine is set currently. The G53 X zero appears to be where the spindle center and center of the boring tool pockets are in line. The G53 Z zero is the face of the chuck. The confusing thing is where the machine is setup for G28. This is the same as the G53. If I am understanding you correctly, the G28 is both a reference point and also the tool change position. So based on that I have no idea why the previous owner had this setup where G53 and 28 are the same.

    Looking forward, I guess I need to figure out what parameter(s) the G28 settings are in and change these. The X position would be somewhere a 1/2" or so from the axis home (full back) and the Z position would be back (Z +) an amount I determine to be a safe distance, taking into consideration what my longest part will be from chuck face + my longest tool. Getting the G28 to correspond to the reference tool is a bit confusing still. If I keep adjusting the parameter for G28 to make the Z display read zero when tool 1 is touched to chuck face, and if I cut a piece of stock right to 1.0" dia. then the X display should read .5" - doesn't this change where my G28 reference position actually is?? I guess I really like the concept you have outlined and are helping me get to, I'm just fully understanding it yet. Thanks for the help thus far!



  8. #8
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default

    Face The Part With A Preset Turning Tool And Set G54 Z Zero At That Point. In Most Lathes You Will Not Need An X Offset.

    Kc
    Application Engineer For A Mori Seiki Dist.



  9. #9
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    MM4039,
    I think I understand your confusion about the reference point. I also suffered that same confusion. I think it might be best to imagine the G53 X0Z0 as a "derived coordinate" which has a relative offset from the G28 position. When we home the machine, it goes to the G28 position, whose display coordinates are preset in parameters. Once the G28 position is reached, this in effect defines where the G53 X0Z0 must be. That is not saying that the G53X0Z0 is at the G28 position. But it does have a well defined offset from that G28 point.

    Whether the machine was ever set up correctly so that the reference tool position is correctly described in the G53 coordinate system, is what I strove to accomplish. Before I did this, the G28 coordinates on my machine were just "tape measure coordinates", not really anything to be relied upon.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    i am very familiar with the fanuc 10t, how i set up all of my lathes is first home out the machine, go into the relative position screen and zero x and z values (origin key on my 10t) i use the face of the chuck as my reference point so i bring the tool down to the chuck and the z value in the relative, will be a negative number, and you manually enter that number into the z column in the geometry offset page. for x i take a cut or position the tool tip on a known diameter and add that to the x value in the relative position, and input that into the x value on the geometry page. so in z that number in the geometry reflects the distance between the tool tip at home position, and the face of the chuck, and in x, the distance between the tool tip in home position and the centerline of the spindle, now to set the g54 go to the work offset page and on both of mine there are 4 sets of values here, #00 is shift,or g53, the numbers in the x,z,and c-if you have it must be zeros in all. next are #01-g54, #02-g55, and #03-g56, all the x values in all the columns set at zero, there should be no reason to change them, now the number you put in the z value of the g54 column will be the distance between the face of the chuck and the finished face of your work (or where z zero in the program will be). the g55 and g56 i use when i have a part i need to flip and want to program both sides at z zero, example: if the g54 is 3.100", and the g55 is 3.050" i will run the first side of the part with the g54 (insert the g54 in the line directly after the tool change of every tool) and programed from z zero, flip the part, then pick up the g55 offset and you have .05 facing stock for the second side of part, in that instance the g55 would be the finished length of the part. on this control you cant change the value of the g54 by trying that in mdi, what you programmed told the machine to pick up the g54 offset, if it was zero the machine understood it as wherever the tool was touched off at, and g1 and g0 are modal commands, they are in effect until it is changed and you dont need to type them in every line for them to be in use. and when it read x0 z0, it was moving to where the tool was touched off at in both axes. there are a lot of ways to set the tool geometry, ive seen a shop that leaves the g54 at zero and touches every tool they use off in z on every part they setup. if anything is unclear please let me know i will explain it differently, i run 2 machines now with the 10t control



  11. #11
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    and i think i was unclear about my x teaching, example: say i take a skim cut and the diameter after was 3.050" and in the relative position for x was the number -15.956", the number i would put in the x column in the geometry page is -19.0060, you moved minus in x to get to the position you skim cut, and you need to add the diameter you turned to that negative number to get to the spindle centerline.



  12. #12
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3086
    Downloads
    0
    Uploads
    0

    Default

    Soooo... in G54 T1 will be at X0 at the theo centerline. So what do you do when you switch to T2?
    I would assume that you continue to use G54 with a calculated tool offset -like- M6, T2, H2 (sorry, VMC lingo) right?

    Setup guy is to be here to set parameters and give me the run through today. I hope everything is good, I have a couple of weeks of work on backlog for it.

    www.integratedmechanical.ca


Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed